Ctrl+K

3D Solid Mechanics

4. 3D Solid Mechanics#

The equations of elasticity describe the deformation of solids due to applied forces. The treatment by the finite element method is very similar.

from netgen.occ import *
from ngsolve import *
from ngsolve.webgui import Draw

box = Box((0,0,0), (3,0.6,1))
box.faces.name="outer"
cyl = sum( [Cylinder((0.5+i,0,0.5), Y, 0.25,0.8) for i in range(3)] )
cyl.faces.name="cyl"
geo = box-cyl

Draw(geo);

find edges between box and cylinder, and build chamfers:

cylboxedges = geo.faces["outer"].edges * geo.faces["cyl"].edges
cylboxedges.name = "cylbox"
geo = geo.MakeChamfer(cylboxedges, 0.03)

name faces for boundary conditions:

geo.faces.Min(X).name = "fix"
geo.faces.Max(X).name = "force"

Draw(geo);

mesh = Mesh(OCCGeometry(geo).GenerateMesh(maxh=0.1)).Curve(3)
Draw (mesh);

4.1. Linear elasticity#

Displacement: \(u : \Omega \rightarrow R^3\)

Linear strain: $\( \varepsilon(u) := \tfrac{1}{2} ( \nabla u + (\nabla u)^T ) \)$

Stress by Hooke’s law: $\( \sigma = 2 \mu \varepsilon + \lambda \operatorname{tr} \varepsilon I \)$

Equilibrium of forces: $\( \operatorname{div} \sigma = f \)$

Displacement boundary conditions: $\( u = u_D \qquad \text{on} \, \Gamma_D \)$

Traction boundary conditions: $\( \sigma n = g \qquad \text{on} \, \Gamma_N \)$

4.2. Variational formulation:#

Find: \(u \in H^1(\Omega)^3\) such that \(u = u_D\) on \(\Gamma_D\) $\( \int_\Omega \sigma(\varepsilon(u)) : \varepsilon(v) \, dx = \int_\Omega f v dx + \int_{\Gamma_N} g v ds \)\( holds for all \)v = 0\( on \)\Gamma_D$.

E, nu = 210, 0.2
mu  = E / 2 / (1+nu)
lam = E * nu / ((1+nu)*(1-2*nu))

def Stress(strain):
    return 2*mu*strain + lam*Trace(strain)*Id(3)    

fes = VectorH1(mesh, order=3, dirichlet="fix")
u,v = fes.TnT()
gfu = GridFunction(fes)

with TaskManager():
    a = BilinearForm(InnerProduct(Stress(Sym(Grad(u))), Sym(Grad(v))).Compile()*dx)
    pre = Preconditioner(a, "bddc")
    a.Assemble()

force = CF( (1e-3,0,0) )
f = LinearForm(force*v*ds("force")).Assemble()

from ngsolve.krylovspace import CGSolver
inv = CGSolver(a.mat, pre, tol=1e-8)
gfu.vec.data = inv * f.vec

with TaskManager():
    fesstress = MatrixValued(H1(mesh,order=3), symmetric=True)
    gfstress = GridFunction(fesstress)
    gfstress.Interpolate (Stress(Sym(Grad(gfu))))

Look at deformed body, use slider deformation in gui controls:

Draw (5e4*gfu, mesh);

The stresses show maximal internal material load:

Draw (Norm(gfstress), mesh, deformation=1e4*gfu, draw_vol=False, order=3);

Exercise:

  • apply loading in \(z\)-direction.

  • look at individual components of stress-tensor (like gfstress[0,0])

Contents